The present invention relates generally to part tolerancing and, more particularly, to an apparatus and method for analyzing the completeness and well formedness of tolerance constraints assigned to features of a subject part.
All manufactured products or parts are subject to variation of their various features, i.e., sufaces, holes, etc., as a result of the manufacturing processes used to create them. The variation in these features compounds as a result of bringing several manufactured parts together to make an assembly. Designers try to control variation by establishing a tolerance plan which specifies how much variation may exist on a particular part. Deficiencies in the tolerance plan, however, often do not become apparent until proto-type pads are constructed, checking fixtures and gages are designed or constructed, and/or pads are manufactured. At this time, changing the tolerance plan can delay production and increase cost. Failure to change the tolerance plan may lead to manufacturing inefficiencies, increased costs and reduced quality. Therefore, it is important to verify early on, while the parts are being designed, that the tolerance plan is well formed.
A difficulty with assigning tolerances to features on a part lies in the measuring of "what" from "where". Often the datum or reference feature from which a tolerance is defined has no relation to the feature being measured. For example, for a given part, an important relationship may be the location of a first feature with respect to a second feature on the pad. The datum, however, may be a third feature which has no importance to either of the two features. Unless the designer is sure to specify the appropriate starting point, the tolerance defined may not be useful. A typical, and unfortunate, reaction by the designer is to simply assign additional tolerances to the features in an attempt to control the important feature. Such practice usually results in inconsistent tolerances, that is, multiple tolerance assignments to a feature which can not physically coexist. In another, and equally unfortunate situation, the designer will not define any tolerances for the feature and thus an acceptable part based on manufacturing variation is not defined.
Thus it is important to have a well defined tolerance plan to identify for the manufacturer an acceptable range of variation for particular features of a part or assembly such that the part or assembly will function as intended. Rules for assigning these tolerances assist in this effort by providing a consistent interpretation of what the designer meant by a particular tolerance assignment. A typical set of rules is provided in the ANSI Y14.5M 1982 standard for Geometric Dimensioning and Tolerancing (GD&T). Unfortunately, even with a rather simple manufactured part, the number of features which may require tolerances can be significant, and the designer has to be assured that each of the tolerances assigned are meaningful, relate in an acceptable manner to each other, and most importantly, allow for the manufacture of a useful part.
The tolerance plan can further be thought of as measurement criteria. The tolerance plan defines what is being measured and from where it is being measured. In this regard, tolerance rules generally require definition of an initial feature or datum from which measurements originate. Based on the datum feature, other features of the part may be defined and measured. Since, however, not all features on a part are of like construction, the tolerance rules also provide for different types of measurements based on particular types of features. The tolerance rules also provide for assigning a magnitude of allowable variation for each of the features assigned a tolerance.
To assist in understanding tolerances it is useful to discuss the concepts of constraint and relaxation and degrees of freedom. These notions were discussed by Bernstein and Preiss in their article Representation of Tolerance Information in Solid Models, Advances In Design Automation, 1989 Proceedings of the 1989 ASME Design Automation Conference, Montreal, Canada, Sep. 17-21, 1989. In designing a part, a designer defines the requirements, for example, the physical dimensions for a mechanical part, in an exact sense. In manufacturing the part, the manufacturer tries to make parts as closely to these requirements as possible, but variation is inevitable. Thus a difficult task becomes defining how much variation is allowable such that the part still functions as intended. In this sense, the requirement or defined feature of the part, for example, the exact location of a hole or the orientation of a surface as specified by the designer, is considered a constraint, and the amount of allowable variation is a relaxation of that constraint.
Constraints are defined with reference to some fixed location and orientation, and under the rules of GD&T defined in the ANSI Y14.5M standard, this fixed location and orientation is called a datum reference frame, and the data used to define the part are called basic dimensions. More than one datum reference frame may exist on a part. Under one interpretation of the tolerance rules one of these datum reference frames is considered a master datum reference frame to which it is desirable to relate the other datum reference frames and features either directly or indirectly. Thus, the features of the part are defined or constrained in space relative to the datum reference frame by basic dimensions. Tolerances, similar to basic dimensions, define allowable amounts of variation for a particular feature with respect to the datum reference frame.
In a pure sense, both basic dimensions and tolerances are constraints because each place a restriction on a relationship of one feature with respect to another feature. Basic dimensions place a fixed constraint on the relationship, e.g., the position of surface "A" is a fixed number of millimeters away from surface "B"in the "X" direction. Tolerances place a variable constraint on the relationship, e.g., the position of surface "A" may vary plus or minus so many millimeters from surface "B" in the "X" direction. For consistency, basic dimensions are referred herein as constraints or constraining data and tolerances are referred to as relaxations or relaxing data. Also, if the tolerances for a particular feature are not properly defined, as specified by the tolerance rule base, it is considered either under-constrained or over-constrained.
Degrees of freedom help the understanding of how tolerances relax constraints in three dimensional space. For example, a cylinder representing a hole through the surface of a part is defined by certain fixed data which identify the location, orientation, size and form of the hole. Variation of some of this data effects the location and orientation of the feature. These are degrees of freedom of the feature. Tolerances permit but also define limits on the amount of variation of the fixed data. Thus the tolerances control the feature degrees of freedom. However, if a tolerance is not assigned, there are a number of possible interpretations. One interpretation is that the feature is perfect, that is, it must be assumed that there is no variation of the data defining the feature or no degrees of freedom. This further implies that there is no variation of this feature on the actual manufactured part, a condition which is not likely. Another interpretation is that large amounts of variation of the feature are acceptable or no control of the degrees of freedom. This, however, is only an assumption, and large amounts of variation may render the part useless.